New to Fanuc Lathe Need Help

[pcast]

First off I am new to CNCzone and hope to be back more often.

Anyway we just got our first CNC lathe and it has a Fanuc 0i mate.

On top of that with my 12 year career it is the first time I have touched a CNC lathe and I am banging my head against the wall.

So what I am trying to is cut 1" x 11.5 NPT that will cut .75" in length.

So I am trying to do my first program by hand is this is what I came up with:

G50
G97 S600 M03
G00 X1.1441 Z0.1
G76 P010060 Q0 R0
G76 X1.1441 Z-.75 R0296 P696 Q320 F0.087
G1 Z0.1
M5
M30

For some reason when I run this program my X travels into the part. Does this have something to do with my Second G76 line.

My back is against the wall and I am about ready to pull the trigger Help!!!!!

[Dan Fritz]

What's with that G50 at the beginning? G50 is an axis preset, and it's usually programmed along with an X or Z. It's also used to specify a maximum spindle speed with an S command, buy you've got CSS turned off with G97.

If you turn on single-block and step through the program, what does the X and Z position display show just before you call that first G76 block?

[BlueChip]

Not sure what you mean by "my X axis travels into the part" but if you mean the taper is going the wrong way ... change the R on the 2nd line to a negative ... I know, sounds dumb but in some Fanuc controls, thinking is backwards.

If not ... please provide some additional info ... hope this helps.

Real World Machine Shop Software at
www.KentechInc.com

[davidw731]

Your X starting point and ending point are the same. Your go X1.1441 should be the major dia of the thread or larger. The G76 X1.1441 should be the root dia of the thread. The number of passes will be calculated by the control using the Q on the second line.

[g-codeguy]

So what I am trying to is cut 1" x 11.5 NPT that will cut .75" in length.

So I am trying to do my first program by hand is this is what I came up with:

G50
G97 S600 M03
G00 X1.1441 Z0.1
G76 P010060 Q0 R0
G76 X1.1441 Z-.75 R0296 P696 Q320 F0.087
G1 Z0.1
M5
M30

For some reason when I run this program my X travels into the part. Does this have something to do with my Second G76 line.

My back is against the wall and I am about ready to pull the trigger Help!!!!!

First of all the X-starting position cannot be the same as the X-ending position in the G76 cycle. Approach X-dimension must clear the part. Second at Z.1 you are giving the machine barely one revolution to get the Z-axis up to speed. Depending on the machine, it can do it at that RPM, but I definitely would back up to Z.3 unless Z0 is not the face of your part. R-value can use a decimal point.

Based on what I see of your program, my guess is that you are trying to machine an I.D. thread.

Try this:

G97 S600 M03
G00 X1.1 Z0.3
G76 P010129 Q30
G76 X1.2644 Z-.75 R.0327 P696 Q200 F0.087
G0 Z0.5M5
M30


Q30 sets minimum DOC to .003. R.001 in the first block would set the DOC for the last pass to .001. 60 cuts on the front of the insert only. I use it when chatter is a problem. I use 00 when there is thread relief. Otherwise I use 01 so the tool can pull out at its fastest.

EDIT: If you feel the first pass is too heavy, but the number of cuts is about right, then make the P-value larger. Making the Q-value smaller will cut less on the first pass, but will increase the number of passes by more than if you lie to 'P'. It can be quite a few more passes depending on how much you change 'Q'.